[henvic]

Hi, I want to run a single-stage compressor calc in Fluent. I.e. a rotor and stator, separated by a mixing-plane.

Both are meshed with TurboGrid and the rotor has a 1% shroud tip gap.

My issue
When I export the rotor mesh to fluent (both using ICEM as an intermediary and exporting as CGNS file), there are 2 vertical surfaces in the shroud gap (shroud-tip-ggi-side-1 and shroud-tip-ggi-side-2). Picture included as attachment.

My Question
How do I get rid of those?

So far I have tried:
- The 'fuse' option in Fluent --> This leads to an error because the no. of nodes in each interface is different.
- Setting them as interfaces --> Lead to numerical error.


Thanks in advance

[Far]

Originally Posted by henvic

- Setting them as interfaces --> Lead to numerical error.

set them as periodic interfaces, but do it in interface panel. No need to make one-one periodic

[AtoHM]

Hi,
If you have a closer look at the mesh, you will see there IS a non-matching interface between the mesh on the suction and pressure side created by ATM meshing. You can prevent having this by employing the traditional meshing technique offered by Turbogrid. This will probably need some more time to set up the mesh, but for blades with a low stagger angle, this can be easily done.

[henvic]

Originally Posted by Far

set them as periodic interfaces, but do it in interface panel. No need to make one-one periodic

Hi, thanks for your reply.

Would it just be a rotational periodic boundary condition with 0° offset? Also, not sure what you mean by one-one periodic. Could you elaborate please?

[henvic]

Originally Posted by AtoHM

Hi,
If you have a closer look at the mesh, you will see there IS a non-matching interface between the mesh on the suction and pressure side created by ATM meshing. You can prevent having this by employing the traditional meshing technique offered by Turbogrid. This will probably need some more time to set up the mesh, but for blades with a low stagger angle, this can be easily done.

AtoHM, is the 'traditional meshing' similar to the manual blocking setup that can be done in ICEM?
How easy is it to increase/decrease cell count whilst maintaining the grid topology? I will probably need to run a lot of different meshes.

[AtoHM]

I am not sure about ICEM, since I did not use it myself. A colleague used it so I would say setting up the mesh is ATM < Traditional < ICEM in terms of time consumption.

The traditional meshing is performed on control surfaces called layers which are created automatically. Depending on the topology you choose (H-,C-,J-Grid) the general distribution is fixed. Then, you can manually adjust the mesh in some regions by using control points at these layers.

To answer your specific question: most values can be adjusted directly in the options. For example, these layers are themselves split in topology blocks, which have a fixed number of cells along each side. This is where you could easily adjust the resolution of your grid. Same options are available for spanwise resolution of the mesh. I would say, if you want the general topology to stay fixed and change only amount of cells, this is a perfect way to do so. I do not know how hard that is to do with ICEM, though.

I attached two images. You can see part of such a control layer and how fine the mesh is depending on the global edge split parameter. Also see number of elements in the left corner. The yellow blocks seen in the grid are changed by this. However the general topology remains the same. To have a matching tip mesh, you need to use H grid at in- and outlet.

[Far]

Here is the process I have applied for Rotor 37 with non matching interface in tip region

[Far]

Here are remaining images

[Far]

But I would like to say, why you are trying it in Fluent. Better option is CFX.

[henvic]

I already have a validated stator model in Fluent so I am building on that.

[Far]

Originally Posted by henvic

I already have a validated stator model in Fluent so I am building on that.

Fluent is perfectly fine for this as well as underlying physcis and equations are same.

Only thing is that CFX gives the solution with few hours for any case for turbomachinery and it has more models.

[Nitrox416]

Hi I am experiencing the same issue,
as suggested I tried the periodic coupling but the solution has numerical problems. I tried in changing the meshing method but didn't succed in finding the correct way to change method in turbogrid.
There is some other method to couple the to tip-shroud wall created in fluent?
Thank you very much

[ersoflow]

Originally Posted by AtoHM

I am not sure about ICEM, since I did not use it myself. A colleague used it so I would say setting up the mesh is ATM < Traditional < ICEM in terms of time consumption.

The traditional meshing is performed on control surfaces called layers which are created automatically. Depending on the topology you choose (H-,C-,J-Grid) the general distribution is fixed. Then, you can manually adjust the mesh in some regions by using control points at these layers.

To answer your specific question: most values can be adjusted directly in the options. For example, these layers are themselves split in topology blocks, which have a fixed number of cells along each side. This is where you could easily adjust the resolution of your grid. Same options are available for spanwise resolution of the mesh. I would say, if you want the general topology to stay fixed and change only amount of cells, this is a perfect way to do so. I do not know how hard that is to do with ICEM, though.

I attached two images. You can see part of such a control layer and how fine the mesh is depending on the global edge split parameter. Also see number of elements in the left corner. The yellow blocks seen in the grid are changed by this. However the general topology remains the same. To have a matching tip mesh, you need to use H grid at in- and outlet.

Hello everyone and AtoHM.

Thankyou for introducing preventing non-matching tip mesh in TurboGrid.
I am not experienced in TurboGrid and I am trying to prevent non-matching shroud tip mesh for my rotor 67/rotor37 analysis in which the mesh will be transforment to openfoam (curently its done for nonTipGap).
I kindly ask you to explain a bit more details about the settings for preventing non-matching tip mesh.

Regards.

[Nitrox416]

Originally Posted by ersoflow

Hello everyone and AtoHM.

Thankyou for introducing preventing non-matching tip mesh in TurboGrid.
I am not experienced in TurboGrid and I am trying to prevent non-matching shroud tip mesh for my rotor 67/rotor37 analysis in which the mesh will be transforment to openfoam (curently its done for nonTipGap).
I kindly ask you to explain a bit more details about the settings for preventing non-matching tip mesh.

Regards.

Hi finally I solved the problem in fluent. You have to change the boundary type from wall to interface and then simply "match " the interfaces with the menu mesh interfaces

[ersoflow]

Originally Posted by Nitrox416

Hi finally I solved the problem in fluent. You have to change the boundary type from wall to interface and then simply "match " the interfaces with the menu mesh interfaces

Hello Nitrox.

Thanks for your answer.
Let me explain myself clearer. I need only the mesh from Ansys side.
When I obtain proper mesh which means "with matching tip mesh" , I will transform it to openfoam then solve it on openfoam.
As far as I know changing the mesh not a way of action of fluent.
The way you told might work for solving the problem on fluent.

What I need is generating a mesh for rotor67 with matching tip gap mesh on Turbogrid.

Regards.

[Nitrox416]

Originally Posted by ersoflow

Hello Nitrox.

Thanks for your answer.
Let me explain myself clearer. I need only the mesh from Ansys side.
When I obtain proper mesh which means "with matching tip mesh" , I will transform it to openfoam then solve it on openfoam.
As far as I know changing the mesh not a way of action of fluent.
The way you told might work for solving the problem on fluent.

What I need is generating a mesh for rotor67 with matching tip gap mesh on Turbogrid.

Regards.

Ah ok I have understand now, I think I can't answer so.
Good luck

[dk9]

Originally Posted by Far

set them as periodic interfaces, but do it in interface panel. No need to make one-one periodic

hi, what kind of interface should we set (rotational, translational)? moreover, which values of pressure did you use for the inlet and outlet boundaries?

Thank you in advance.